Help needed for advanced homework.

[Anonymous]

Hi.

I just got this paper handed out that's due this friday. I like to start early on these things, and although I feel like I don't have too much time for this particular assignment, I couldn't have started any sooner.

I'm not looking for someone to do this assigment for me, I'm just looking for some helpful tips, and a walkthrough would be perfect but I doubt anyone has got the time for that. 

The problem for me is that I haven't used inventor before. We started using it on school two weeks ago and I've done all the exercises, but this seems beyond me. Any help as to where I should start, how I should do it etc would be immencely appreciated.

Right now I've done part 6 just to get started, and I'm starting on part 6. I'm unsure as to where to begin..

Any help and discussion appreciated!

Edit: I'm using Autodesk Inventor 2013 professional.

Edit 2: If there's a problem with the language, I'll be happy to translate whatever you need to understand it instantly. I just figured the images and measurements should be enough, but I clearly understand if anyone has any questions about the other text. I'll obviously answer any other questions as well related to this.

Edit 3: Any feedback is appreciated. If there's something wrong about this post, the info I'm giving etc. 

[Anonymous]

Ahh, that makes sense. Was trying to do this too quickly, getting carried away here!

I've now finished part 3, and moving on to part 4. Attaching part 3 here.

[JDMather]

You might want to use diametral dimensions rather than radial.

It is no more effort.

Click the center line rather than then end of the center line.

One advantage - when creating 2D drawings you will want the diameter rather than radius dimension and you can retrieve the dimensions from the model.

Save steps.  Get lazy!

You are doing very well on this.

Most students that come here don't stick with the assignment to completion.

When you get a chance I recommend you go through these

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf
http://inventortrenches.blogspot.com/p/inventor-tutorials.html
http://wikihelp.autodesk.com/enu?adskContextId=HELP_TUTORIALS&language=ENU&release=2014&product=Inve...

[Anonymous]

I'm sorry, I don't understand what you mean here. Which dimentions are you talking about? I though all my dimentions were diametral. 

Well, I feel I'm learning a lot, and that's the most important part. I came in here being frustrated that I hadn't learned enough to complete this assigment myself and I really didn't like inventor. Now I think it's exciting, I'm working A LOT faster and I actually understand a lot of what I'm doing. It's a great feeling, and I'll continue to work on this until I'm completely done even if I can't hand in the whole assignment in time. That's how much I enjoy doing this now.

Well, I'll continue working as long as you guys review my progress heh. That's what makes it interesting I guess, and hopefully I don't waste your time.

[CCarreiras]

Hi!

It means, if you are using the "center line", you can use it to have diameter dimension instead radius dimensions, and later, when you go to the drawing, you can use this "sketch dimensions" to document the drawing using the tool "Retrieve dimensions"!!! Half of the work!!!

Try it!!! Delete the "4" dimensin and add the "10" for diameter as you see in the picture.

TIP: use the dimensions as you have in your home work document, it's easear to follow any errors.

[Anonymous]

Alright, thank you! I've got it now I think. Attaching part 4 as well since that's so small. 

If everything looks well now, I'll move onto part 7.

Also, I will be checking out the links in the post above for sure! I really appreciate that. I just want to get this assignment out of my head first, it's taking up a lot of my focus!

[Anonymous]

All looks well in Part 3 except for your hole.  You do not have it fully constrained (Sketch).  Be sure to use Constraints and Dimensions where needed.  For that one, I would use the Coincident Constraint on the Point and the Projected Origin XY Plane.  You will need to turn on the Origin XY Plane and Project it in your sketch.  Then use the Coincident Constraint for the Point and the Projected Plane.  This ensures your hole will always be in the middle of your part regardless if the parts overall shape changes.  Next you need to dimension the point along the shaft of your part. This will fully constrain your hole and allow you to change the location with ease if the need arises.

[JDMather]

Part 3 the hole location is not fully defined.

Add the dimension (it must have been there?) and a horizontal construction line or a horizontal constraint to the origin.

[Anonymous]

I'm sorry Dan, I didn't understand what you meant. I will look into it later though, I can guarantee you that. Now I'm looking forward to do part 7.

Thanks a lot for your help!

[JDMather]

The real fun comes when you get the assembly put together and it works!

[Anonymous]

No problem.  In your newest part, you now have the hole (Sketch 2, Extrusion 1) properly constrained.  In your previous Part, the hole was free to move about in any direction in your sketch.  There was no constraints or dimensions.  I was trying to explain how to constrain the point (your hole) properly.  You have seemed to fix that and it is now properly constrained and sketched. 

When it comes to sketches, always try to think of this... "hmmm if my boss wants to change the shape of this part or change the location of a feature, how can I do so in such a way that will make things easier?!"  By always planning for the worst (ie parts changing) it will save you hours later down the road!  You are doing a great job and the parts seem to be "JD Worthy" so give yourself a pat on the back.  When this is all said and done, as an exercise, you should re-do the entire project and see how far you have become. 

[Anonymous]

I will look into your reply asap Dan, I just have to get this out of my head first. 

I was editing my above post when I got timed out unfortunately.

I've started part 7, and I feel like I'm lazy, but I'm already stuck. I can't figure out how to make the big hole properly. Extrude hole didn't work, obivously. Also, the little hole was tricky as well. I tried making a circle in my original sketch, and then revolving it, but as I did this I looked at the assignment, and it should only be a 'tap' on one side, and not fill the whole space on part 5. Maybe I can make a new sketch on top of the bottom of my existing model, then extrude a circle/arc? I'll try that.

I'll obviously attempt myself while I wait for your inputs, and if I come up with something, I'll edit my post.

[JDMather]

Do not Extrude a circle for the hole.

Start the Hole feature command.

Set Concentric as the placement method and then select the planar face and then the cylindrical face.

(and why didn't you use diametral dimensions in the first sketch?)

[Anonymous]

Thanks!

I told you I was getting lazy. I'll wrap this up now and hand in what I've got so far, then call it a night. I'll post here when I continue my work on inventor tomorrow evening. That way I'll avoid wasting your time because of my careless mistakes.

Thanks again for all your help today, I've learned a lot! I really appreciate it.

[Anonymous]

Alright, I'm back after a busy day.

Dan, I get it now. I was having trouble turning on Origin XY Plane and Project in my sketch. Thanks for showing me this, I'm sure it'll be useful for the next assignment, and it'll be usefull whenever I'll use inventor in the future anyways. I'll do my best to implement this.

I've now done a 2nd attempt at part 7 (started all over again) with a little more focus and concentration and a little more effort I hope. Thanks to your help, JD, I think I've done ok this far, but that lock pin (this is where my technical English fails me) - I don't get it! 

My idea was to make a circle and extrude cut, but I can't figure out how to make the circle on the right plane so to speak. I'm only able to make a sketch on the same plane as my hole if you understand.

[JDMather]

Expand the Origin folder in the browser and right click on the XY plane to start a New Sketch. (it doesn't really matter if whether you pick the "Front" plane (XY) or the "Right" plane (XZ) for this hole feature becuase the part is cylindrical.

Then hit F7 on the keyboard for improved visibility while creating the sketched circle.  (this will temporarily slice your model in half).

After dimensioning the size and location of the circle, Extrude-Cut mid-plane, through all.

See attached.

[JDMather]

or you could edit Sketch1 to add the circle and then make it Visible and Extrude-Cut.

But I recommend you try the first method I suggested to learn something new.

You are almost finished.

You are really going to like this when you get it assembled.

You will assemble one "finger" with the fastening parts to the "yolk" (not sure what you would translate these to from your drawing), and then pattern the other two.  We can also get the screw rotating/moving as expected.

[Anonymous]

Thank you.

I tried the first method. The F7 'tool' is great to get a better view of the part, at least in this particular case. When it comes to placement, I just used tab to enter distance from the x and z axis.

I hope this looks ok now, and I'll be moving on to part  2 and 9 and it looks like I'll have all the parts ready to assemble. I'm getting excited for that!

[JDMather]

You are making up dimensions again - and have not dimensioned the hole location correctly.

[Anonymous]

Which dimensions am I making up? The small hole I had to use the auto dimensions and constraints to be able to extrude it because I couldn't figure out how to do it otherwise. I can't say I understand some of the constraint functions, and that's sort of bugging me. 

I've now just added two dimensions to show how I was thinking when I was placing the small hole. 

[JDMather]

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...I had to use the auto dimensions and constraints ...

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Forget forget forget you ever saw that tool.